Differing results with closed corners

[HDEAR]

I get differing results using 'Sheetmetal Closed Corners' when I use 'Bends', 'In bends' and 'Out bends'

 

'Bend' works perfectly but often I would rather use 'In bend' or 'Out bend' depending on what type of sheetmetal construction I am working on,purely to save time having to make bend and material thickness allowance calculations.

 

The following pictures describe the problem.

 

First picture shows what result I get when using 'Bend', then closed corner. Happy camper with this one.

 

Using 'In bend' and 'Out bend', once I perform the bends, one overlaps the other, so it needs to be brought back so that the indices match. This is where the problem seems to begin - refer second and third pics and you will see material left over from moving the bend.

 

Then when I apply closed corners, there is material left in the corner which is not what would happen when making such a bend in reality.

 

Is it possible I have to add some sort of relief before performing the move bend for in and Out bends? If that was the case, then wouldn't that defeat the convenience and purpose of using 'Closed Corners'?

 

Any advice welcome, thanks - Harley

Edited October 11, 2014 by HDEAR

[jolizon590016]

Any update from the community on this or closed corner on applies to bend only.

 

regards - joseph

Edited October 18, 2014 by jolizon590016

[Jonas@Solidmakarna]

I usually never use the In our Out Bend shapes, the issue mentioned above is one reason.

 

Another reason is that the size of the part should be set after you've made the principal "shape" of the part.

 

So just drag out the features needed, then go through the dimensions, it is much faster and easier. Though probably not how people are used to think and that is why this question usually comes up. Also make sure that you have the Options, SheetMetal setting "Auto-Constrain bends" active, so that everything follows when you change the dimensions.

 

When working with SheetMetal in IRONCAD you should use the Shape (profile) handles. They are really great and work in all situations everywhere.

 

You can have a look at this video (from 40s), I hope it helps eventhough the built in video comments are in Swedish -

 

[HDEAR]

I usually never use the In our Out Bend shapes, the issue mentioned above is one reason.

 

Another reason is that the size of the part should be set after you've made the principal "shape" of the part.

 

So just drag out the features needed, then go through the dimensions, it is much faster and easier. Though probably not how people are used to think and that is why this question usually comes up. Also make sure that you have the Options, SheetMetal setting "Auto-Constrain bends" active, so that everything follows when you change the dimensions.

 

When working with SheetMetal in IRONCAD you should use the Shape (profile) handles. They are really great and work in all situations everywhere.

 

You can have a look at this video (from 40s), I hope it helps eventhough the built in video comments are in Swedish -

39177[/snapback]

Thanks so much Jonas. I have been working in sheetmetal for over 40 years now so making the calcs for bends and lengths is second nature. I guess I was feeling lazy seeing that in and out bends were a feature and theoretically could save a bit of time, but seeing they cause that much trouble I'm fine making the calcs or as you say finish the basic shape and work from there.

 

The 'Auto-constrain bends" is active, I just checked. I'll do more experiment with shape handles as see what I can dream up.

 

Again, so grateful for your input.

 

Harley

Edited October 16, 2014 by HDEAR

[mwalls558626]

Have to chime in just a little on this one. I do a lot of sheet metal parts, and I don't worry about what type of bend I use to build my part, because I want to take advantage of how the InBend, and OutBend work as I am creating the sheet metal part using other existing geometry as reference points. If you have the Auto Constrain on that bend, which is a good default most of the time, you will have to drill down to the intellishape level of the bend, Right Click on the blue constraint that will be showing for the bend, and "Unlock" the constraint of the bend so you can "pull back" the stock material without moving the entire bend feature. The constraint will be there if needed later, just not locked.

 

So what I do is build my sheet metal part using whatever bend type I want, then go back to the corners and check to see if they have any extra stock there, and if they do, I unlock the constraint on the bend, and pull the base material back to the tangent point of the bend radius. More often than not, all you will have to do is pull back one side, and it will, by default, correct for the 2 sides perpendicular to that bend if they are an issue.

 

Mike

[HDEAR]

Thanks Mike for chimimg in and bringing up the awareness of the constraints. So much to learn and so little time

 

I couldn't find the 'blue constraint' at the intellishape level of the bend however when I changed 'Options-Sheet metal-Constraints - Auto constrain' to off, it worked.

 

Just to make sure I am doing this right, I left clicked on the bend twice to bring up the intellishape level ( yellow dotted lines ) but when I hovered over all the handles, none were blue, they were all yellow. Bet I'm doing something wrong or missing a point because I would like to be able to change auto constrain on the fly, rather than have it globally set for the whole scene parts.

 

UPDATE! Solved it. The blue constraint appears under the shape control. I right clicked that and it come up with menu that did not mention 'Auto constraint', but had the option 'Lock'. Once I un-ticked 'Lock' I could do what you mentioned. Obviously this 'Lock' refers to the constraints.

 

Pics below

Edited October 25, 2014 by HDEAR

[mwalls558626]

Yes, that is exactly what I was trying to explain. Good job figuring it out. It is not always easy to put down verbally, something that is so visual! I hope that works well for you.

 

Mike

[HDEAR]

Yes it has thanks. I've managed to put out two new designs and have them produced by our contract sheet-metal fabricator. Even had to learn about producing drawings and saving them in .dwg as they only have autocad 2004 !!! On to the next challenge I guess...